SZGH SZGH-CNC1000MDb Series, Руководство пользователя

Страница: 72 / 223

-Shenzhen Guanhong Automation Co.,Ltd.- SZGH-CNC1000MDb Series
- 59 -
the tool center moves as in (2), and vice verse. Consequently, the same tape permits cutting both
male and female shapes, and any gap between them can be adjusted by the selection of the offset
amount. Applicable if start-up and cancel is A type.
Fig3.20.4 Tool center paths when positive and negative tool compensation values are specified.
Note: 1. The tool compensation value corresponding to offset No.0, that is, D0 always means 0. It is
impossible to set D0 to any other offset amount.
2. Tool compensation C can be specified by D code.
3. Setup & Cancel of tool radius offset C are set by P1 & P2 on tool parameter.
The offset vector is the two dimensional vector that is equal to the tool compensation value
assigned by D code. It is calculated inside the control unit, and its direction is updated in
accordance with the progress of the tool in each block. The offset vector is deleted by reset.
Specify a tool compensation value with a number assigned to it. The number consists of 01 to
99 after address D (D code). The D code is valid until another D code is specified. The D code is
used to specify the tool offset value as well as the cutter compensation value.
Offset calculation is carried out in the plane determined by G17, G18 and G19, (G codes for
plane selection). This plane is called the offset plane. Compensation is not executed for the
Coordinate of a position which is not in the specified plane. The programmed values are used as
they are. In simultaneous 3 axes control, the tool path projected on the offset plane is compensated.
The offset plane is changed during the offset cancel mode. If it is performed during the offset
mode, CNC system will alarm and stop moving.
Example:
G54 X0 Y0 Z0 ; ........................................Specifies a workpiece coordinates system.
The tool is positioned at the start position (X0, Y0, Z0).
N1 G90 G17 G00 G41 D03 X250.0 Y550.0;
Starts tool compensation(start-up). Tool is shifted to the
left of the programmed path by the distance specified in D03.
In other words the tool path is shifted by the radius of the tool
(offset mode)Because D03 is set to 15 beforehand(the radius of
the tool is 15mm).
N2 G01 Y900.0 F150 ; ...................................Specifies machining from P1 to P2.
N3 X450.0 ; ....................................................Specifies machining from P2 to P3.
N4 G03 X500.0 Y1150.0 R650.0 ;..................Specifies machining from P3 to P4.
N5 G02 X900.0 R-250.0 ;...............................Specifies machining from P4 to P5.
N6 G03 X950.0 Y900.0 R650.0 ;...................Specifies machining from P5 to P6.